Ansys meshing with extended meshing
I recently installed ansys 13 in my system. Till now I am using gambit -> Tgrid -> fluent for my analysis.
I came to know that in ansys 13 onwards, we can use Tgrid or ICEM CFD interactive mode in ansys meshing. So I tried to use workbench to automate the analysis. But I faced some difficulties
1. My geometry has rotational periodic faces. So It can be meshed only with patch dependent method in Ansys meshing. But ICEM CFD interactive mode (Extended meshing) is not available for patch dependent method. so I could not edit the mesh and improve the quality. It is very important for me.
2. Then I decided to use Tgrid interactive mode. I gone through help and found that also not possible for me. Because it will only work for cut cell method.
There is any way to use ansys workbench wih models have periodic faces in the goemetry? Or am I missing some thing?:confused:
In Workbench it allows the Interactive modes of ICEM and TGRID for methods coming from ICEM or TGRID. For TGRID this is Cutcell for ICEM it is PI Tetra and Multizone.
There are two types of Interactive mode:
Back to your specific problem I can think of a way to do what you want manually but not automatically with the PC Tetra method.
You could use the PI Tetra method, but over ride the mesh generation so it just brings up ICEM CFD. Load the starter replay file and go down to the indicated line... Then begin. You can setup the periodicity in ICEM CFD and it will be recorded in the script... Then mesh the model with any ICEM CFD method you want (maybe start with PI tetra, then do a delaunay TGLib fill and insert prisms), edit the mesh, smooth it, what ever. All will be recorded in the replay script.
In the end, quit ICEM CFD, save everything when it asks you. It will suck the mesh back into ANSYS Meshing. Then switch from ICEM CFD interactive to ICEM CFD Batch. From now on, updates will re-run the script instead of popping up interactive ICEM CFD...
By the way, this also works in 2D if you use the aligned quad method.
Hello Simon and Sac,
Thanks for your suggestions. I think that I can use workbench for my analysis.
Simon: I have few queries in workbench. Please clarify this.
1. If I use ICEM CFD Extended meshing, in some areas I will ignore the geometry (slightly) to improve the quality. But ansys meshing is geometry dependent. At this situation, ansys meshing will take the mesh from ICEM CFD correctly?
2. If I define the boundary type for periodic faces (Named Selection) in ansys meshing, this is not exported to fluent. Only boundary names are exported to Fluent. I am manually setting the periodic boundary condition in Fluent.
Also for each parameter changes, I am getting this error for periodic boundary setup. After setting manually, Fluent solves the analysis. How to overcome this?
Expecting your reply
1) The attachment in ANSYS Meshing does do a mesh quality check and a topology check (to make sure the mesh surface patches match the geometry surface patches). So yes, if you really went patch independent, your attach could fail... Some slight fudging may be OK. Honestly I have not played with it enough yet in 13.0 to get a good feel for how far I can push it.
2) I will mention this to someone and see if they plan to fix it...
Thanks for your prompted reply. I will also try to use ICEM CFD extended meshing and check how much it works well with ansys meshing.
Many times you helped me when I am facing some critical issues. Now you replied to me in week end also. Generally tech support also not available in week ends:p
Thank you very much:)
I am not tech support ;)
I actually do most of my CFD-Online outside of work hours...
When I do log in during work hours, my main justification for being here is to keep an eye on what you guys are struggling with and use that info to plan development tasks...
|All times are GMT -4. The time now is 06:12.|